I am just getting started on PCB design (for fun) and came across this term called thermal relief. It increases thermal resistance so the components can be soldered easily. But according to what I have learned, thermal and electrical resistance are always connected. So does thermal relief in any way increase the electrical resistance also? If not, what is the mistake I am making? This may sound silly but I cannot get it out of my mind.

  • 2
    \$\begingroup\$ The four traces are at least big as an ordinary trace. You're just not getting the full 360 degree connection to the ground or power plane. But if there was no such plane, you would only have a thin trace. The thermal relief is used because the conductance of heat is so good that it's difficult to solder the pad. That also means that electrical conductivity is ridiculously good; more than you usually need. \$\endgroup\$
    – Kaz
    Commented Jul 19, 2013 at 18:57
  • 4
    \$\begingroup\$ A more interesting question might be if it adds enough inductance to be significant in high speed applications. \$\endgroup\$ Commented Sep 20, 2013 at 15:33
  • 1
    \$\begingroup\$ "thermal and electrical resistance are always connected" Not necessarily: Diamond is an electrical insulator and the best solid thermal conductor known. \$\endgroup\$
    – endolith
    Commented Sep 6, 2016 at 21:58

3 Answers 3


A thermal relief pad is essentially a pad which has fewer copper connections to a plane (such as a ground plane).

A normal pad would simply be connected in all directions, with the solder mask exposing the area to be soldered. However the copper plane then serves as a giant heatsink which can make soldering difficult, because it requires that you keep the iron on the pad longer and risk damaging the component.

By reducing the copper connections, you limit the amount of heat transmission to the plane. It follows of course, that with reduced copper conduction paths, you also have greater electrical resistance. The increase in resistance is marginal compared to the reduction in thermal conductivity.

This should not be a concern unless the pad is carrying high current such that the four traces (on a standard thermal relief) together are insufficient to carry the current; or if it is for high frequency signals where the thermal relief may cause unwanted inductance.

Just to show a visual on normal vs thermal relief pads:

Normal vs Thermal Relief PCB Pad

The pad at left is connected to the copper plane (green) in all directions whereas the pad at right has had copper etched away such that only four "traces" connect it to the plane.

Just for fun, I used a trace resistance calculator to estimate what the electrical resistance difference might actually be.

Consider the thermal relief pad. If we assume the four "traces" to be 10 mil wide (0.010") and approximately 10 mil in length from the pad to the plane, then each of them has a resistance of about 486μΩ.

The four "resistors" in parallel would give us a total resistance of :

$$R_{total} = \frac{1}{\frac{1}{486\mu\Omega} \cdot 4} = \frac{486\mu\Omega}{4} = 121.5 \mu \Omega$$

If we approximate one empty space created by the thermal relief to have the equivalent of about three such traces, giving us 16 in total:

$$R_{total} = \frac{486\mu\Omega}{16} = 30.375 \mu \Omega$$

Remember these values are micro ohms or \$0.0001215\$ and \$0.000030375\$ ohms, respectively. So by rough estimate, the difference in electrical resistance between our two hypothetical pads is a mere 91.125μΩ.

The thermal properties, on the other hand, are significantly different. I don't know thermal conductivity formulas very well, so I won't try to calculate it. But I can tell you from experience that soldering one versus the other is highly noticeable.

Values calculated assuming a 1 oz copper layer.

  • \$\begingroup\$ That makes since. Its that electrical resistance also increases but the increase is not that significant compared to thermal resistance \$\endgroup\$ Commented Jul 19, 2013 at 8:29
  • 2
    \$\begingroup\$ For thermal calculations, although not precise, you can mostly assume the change in thermal resistance is proportional to the change in electrical resistance. So, your 4x increase in resistance (which, as you said, is still only an incremental increase) gets you on the order of 4x "easier" soldering. The thermal equations bear a striking resemblance to the electrical ones. \$\endgroup\$
    – scld
    Commented Sep 20, 2013 at 16:26
  • \$\begingroup\$ This answer is REALLY good, but you should give a look to this answer to a similar question that makes a lot of sense, so basically depends if your board of gonna be soldered by hand (then you put thermal relief ) or in oven (then you don't put thermal relief). \$\endgroup\$
    – JAMS88
    Commented Jul 18, 2014 at 4:04
  • \$\begingroup\$ +1, awesome answer. Is it true that for a through hole pad a thermal relief pads are necessary only on plane layers (PWR and GND)? On signal layers (bottom and top) there is no need for a thermal relief pad, isn't it? 10x. \$\endgroup\$ Commented Dec 23, 2016 at 9:15
  • \$\begingroup\$ @Segei Yes, a signal layer where the pad connects to a trace rather than a plane should not need a thermal relief. If the trace is large, there may be exceptions. \$\endgroup\$
    – JYelton
    Commented Dec 23, 2016 at 18:29

An additional benefit to the use of thermals is when you need to remove a component from a PCB for replacement or other reasons. It is way more difficult to desolder a lead that is soldered to a pad that has no thermal relief but is tied to a plane or pour. Any person reworking a board that you have designed will appreciate your thoughtfulness for using thermals. In RF work the inductance of the thermal spokes will be negligible until you get to frequencies that are really high, 10s of Gigahertz or better, where markedly different methods of hooking things up are used and vias are mostly used to tie ground planes together (spaced less than one wavelength of the frequency expected apart and stitched all around the periphery of the plane or pour) not to route signals through. (You can always find exceptions to any "rule" if you try, but the last sentence is generally true.)


There are exception to every rule. Good question. Good answers above. I generally use "direct connects" for via and pads to planes. Except if there is a through hole component that needs to be soldered. So for through hole components like connectors, resistors, capacitors etc, if they're connecting to a plane, use a thermal relief. Note a large trace can become a "thermal plane". For SMT components, I use "direct connects" because, I assume, the board is being assembled with reflow in an oven. The oven controls the temperature of the entire board, so a thermal relief doesn't aid in assembly. I don't recommend hand assembly of SMT for reliability reasons. Its relatively easy to crack a capacitor hand soldering it. Even for trained assemblers. Repairing is a secondary concern. Most often the board is scrapped. Or should be.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.